Technical Drawing Training Lesson 8: Dimensional Tolerances and the ISO System of Fits

No part is ever made to its exact drawing size. A dimension of 20 mm really means “20 mm, within a stated margin”. That margin is the tolerance, and choosing it correctly is the difference between a part that assembles and one that does not — or one that is needlessly expensive.

The vocabulary

• Basic size — the main figure written on the drawing (20).
• Upper deviation — how far the actual size may go above the basic size.
• Lower deviation — how far it may go below (or, if positive, the minimum amount above).
• Maximum and minimum size — basic size plus each deviation.
• Tolerance (T) — the difference between them; always a positive number.
• Zero line — the line representing the basic size on a tolerance diagram.

A part is accepted if its measured size falls anywhere between the minimum and maximum size. It does not have to be “close to nominal” — anywhere inside the zone is equally good.

The ISO system: letters and numbers

ISO 286 describes a tolerance with a letter and a number, for example H7 or g6.

• The letter gives the position of the tolerance zone relative to the zero line. Capital letters (A…ZC) are holes; lower case (a…zc) are shafts.
• The number gives the width of the zone — the IT grade. IT01 is the tightest, IT18 the widest. The smaller the number, the tighter the tolerance.

So Ø20 H7 means a hole 20,000 to 20,021 mm. Ø20 h6 means a shaft 19,987 to 20,000 mm. Same nominal size, opposite direction of tolerance.

The three types of fit

On a tolerance diagram the rule is easy to see: if the hole zone lies entirely above the shaft zone the fit is a clearance fit; entirely below, an interference fit; if they overlap, a transition fit.

Hole basis and shaft basis

• Hole basis. The hole is kept at H and the shaft letter is changed to obtain the fit: H7/g6, H7/k6, H7/p6.
• Shaft basis. The shaft is kept at h and the hole letter is changed: G7/h6, K7/h6, P7/h6.

Both give identical fits. In practice the hole basis system is preferred, because a hole is made with a fixed-size tool — a drill, a reamer, a broach — while a shaft can be turned to any size. Changing the shaft is cheap; changing the hole means a new tool.

Shaft basis is used where a single long shaft or a standard drawn bar has to carry several different fits along its length — for example a transmission shaft with a bearing, a gear and a pulley on it.

How a fit is written on a drawing

• On an assembly drawing: Ø20 H7/g6 — hole tolerance first, shaft tolerance second.
• On a detail drawing: only that part’s own tolerance, e.g. Ø20 H7 or Ø20 g6.
• Deviations may also be written directly as figures, e.g. 20 ^+0,021₀.
• Dimensions with no tolerance are covered by the general tolerance note, usually ISO 2768-m.

Worked Example: Ø30 H7/g6 Tolerance Zones

Let us put real numbers on a fit. For Ø30, an H7 hole gets +21/0 µm and a g6 shaft −7/−20 µm. The hole zone sits above the zero line and the shaft zone just below it, so this is a clearance fit: at tightest 7 µm and at loosest 41 µm of clearance — the shaft always enters the hole, never jams:

Test yourself

1. What does the capital letter in H7 tell you?
   That it is a hole, and where its tolerance zone sits relative to the basic size.
2. What does the 7 in H7 tell you?
   The IT grade — the width of the tolerance zone. Smaller number, tighter tolerance.
3. What is the lower deviation of any H hole?
   Zero.
4. Ø30 H7/p6 — what kind of fit is that?
   An interference fit; the shaft is always larger than the hole.
5. Why is hole basis preferred?
   Because holes are made with fixed-size tools; it is far cheaper to vary the shaft.
6. A shaft measures 19,992 mm and is specified Ø20 h6 (19,987–20,000). Accept or reject?
   Accept — it is inside the zone.
7. What governs a dimension with no tolerance written on it?
   The general tolerance standard named in the title block, typically ISO 2768-m.